how to deal with sharp trailing edges in icem
 

Hi,

I am meshing a wing with a sharp trailing mesh (using unstructured meshes), but the quality of the mesh in the trailing edge is very poor (highly skewed elements), I wonder if there is a way to deal with sharp trailing edge.

joel

clarify
 

Unstructured Hexa? Unstructured Tetra/Prism?

2D? 3D?

Check out the web...
 

If it is unstructured hexa, check out www.youtube.com/ansysinc/

Hi Simon,

It is unstructured tetra/prism. I will check the link.

Thanks a lot,


Joel

Prisms
 

Ok, so your issue is probably the trailing edge prisms?

So what do you want it to do? Do you want it to give you wrap around prisms whose internal angle approaches 180 degrees? Or do you want it to step down and avoid the wide angle prisms? Or you could extrude the trailing edge curve back into a surface and run the prisms along that for some distance behind the wing... (The answer to this depends on your solver requirements).

ICEM CFD Prism has many settings, perhaps this ppt will help...

ftp://ftp.ansys.com/outgoing/simon/Prism_NoPyramids.pdf

If not, you will need to post a bit more info (like maybe an image of the cut plane thru the poor quality elements)

Sooner or later I will make a YouTube movie about dealing with sharp 3D wings...

Hi Simon,

Well basically I want to do something similar like in gambit (see figure 4), so I was wondering if there is an option to do that automatically in icem (and sorry for bringing down gambit into an icemcfd discussion).

In figure 1 and 2, you can see what I am actually getting and honestly speaking, I am not satisfy with the quality of the elements close the trailing edge. I already tried with several max prism angles and I still do not like the output.

I also take this opportunity to ask you a different question. Take a look at figure 3. I wonder if there is a way to enforce the mesh on the left side to be identical to the mesh on the right side (so I can impose later on the solver a periodic condition). I also wanted to know, if there is a way to make the tetra mesh grow uniformly, as you can see in this figure, close to the wing the mesh does not grow uniformly respect to the spanwise direction. In gambit I can control this by setting a fixed side function (again, sorry for comparing with gambit), how can I do something similar in icemcfd?



cheers,

joel

the missing attachment

Sure... No problem.
 

To setup periodicity, you can go to the Mesh Tab, first ICON (global Params) and then into the Global Prism Params. You can set up for translational or rotational periodicity. In ICEM CFD you just need to set the offset, you don't need to pic the actual periodic surfaces.

We have a number of ways to get something similar to the last image... You could use MultiZone which would give you a pure Hexa boundary layer and probably sweep between the periodic walls. You could use the geometry tools and extrude the trailing edge back from the curve and just grow prism on it like normal. If this wing is really just 2.5D (2D Extruded), then you could also use extrude to get a swept mesh...

Simon

Hi Simon,

Ok, I managed to setup the periodicity and I get a very nice tetra mesh, but when I add the prism layer, the mesh is not periodic anymore. Suggestions?

Joel

Periodic Prism...
 

Prism should also be periodic... Not sure what has gone wrong...

Does it not look periodic or is it just failing the check? The check fails if the parts are not periodic and I have seen it think a mesh was not periodic simply because of the part names of a curve segment...

Maybe send me the file and I will run it.

Simon

Oops..
 

I had confused your email with another asking me to Hex mesh a wing... So I got your model and quickly hexa meshed it... (I should ask people to include a link to the thread when they email me)

It just takes 3 splits (2 horizontal and 1 vertical) followed by an ogrid thru 1 block with 3 faces... (C-Grid really).

Attachment 3332

Then I split for the trailing edge and collapse the trailing edge block.

Attachment 3333

I then split the front face to associate it with the wiggle front edge, did the rest of my associations, made it periodic, setup sizes, etc. <10 minutes total.

Attachment 3334

Since it is in ICEM CFD Hexa, you can go back into the file and adjust the distribution as necessary.

Do you still want to use tetra prism for this model? if so, I can look into that periodic prism issue.

Yes, an hexa mesh is a better mesh, but the problem is that I was specifically asked to generated an unstructured mesh.

Regarding to the periodic issue, the check does not fail (at least icem manage to generate a mesh), but the faces do not seem to be periodic at all by visually inspecting them (specially the prismatic layer).


Joel

http://www.cfd-online.com/Forums/att...1&d=1274025864I am so excited I finally have a nice 3D cgrid. Only problem is no surface mesh on wing. If I try to split in other ways I get mixed surfaces?

Thanks
http://www.cfd-online.com/Forums/att...1&d=1274025864
Brian

Structured/unstructured
 

To Joel...

Unstructured just means the way the mesh is stored... In the old days, there were many solvers that only handled "structured" meshes which was a very structured way of storing the mesh data and happened to require hexa. Unstructured just means that you store the data as node locations and the elements that contain those nodes. It can be any mesh type. Early versions of CFX and Fluent supported Structured mesh, but the more recent versions have been "unstructured solvers"...

In ICEM CFD you can output a Hexa mesh as Structured or Unstructured. There is no real reason to specify an unstructured tetra/prism mesh when an unstructured hexa mesh would be easier to generate and produce a much better quality result... However, during the next work week, I will still look into your translational periodicity issue with prism.

Simon

Brian,

I am glad you were able to follow those rough instructions. It is important to take smaller steps like this before tacking your final model.

The step I forgot to mention was to delete the wedge block (or at least put it into a different volume material).

Since the wedge is currently the same material as the rest of the blocking, ICEM CFD interprets it as all one volume and the default surface projection between blocks is "none". You can mess with individual face associations, but it is easiest to just delete that wedge block (not permanently, which really just moves it to the VORFN part). Alternatively, if you wanted to look at heat transfer or something that required keeping that wedge mesh, you could just create a new part (SOLID) and add the blocking material to that part.

ICEM CFD would then assume that you wanted boundary elements at the borders of the fluid volume and you would see your airfoil surface.

Best regards,

Simon

I still have few problems to deal with. I made another split for the wing and I have a surface boundary spilling over to another surface, see attached. Then I have these low quality elements, which I dont understand or can't fix. For some reason the edge which comes off the trailing has bad surface elements?? Doesnt show well in pic but it is noticealby thicker. Sorry for not having figured out to resize pics yet.
http://www.cfd-online.com/Forums/att...1&d=1274117717

Thanks

Brian


http://www.cfd-online.com/Forums/att...1&d=1274117830

Prism...
 

Joel,

I tested on this and other models and Prism came out periodic every time... So, not sure what the problem was on your end.

In these pics, I have clicked on the "Z" in the triad (same as "Shift Z" or "view => front") and I am showing all the surface elements... The periodic faces are completely lined up so you can't even see the back face (is this the kind of visual inspection you did?). I also ran the periodic checks and they turned out fine also.

Attachment 3404

Attachment 3405

Looking at your model, I see you set up sizes on curves instead of surfaces. You also didn't take the opportunity for curvature and proximity sizing (like the gambit size function) or the feature to let the prism height float for better transition.

This first image is just changing the "Height limit factor" to 0.7...

Attachment 3406

But this next picture is with all my own settings...

Attachment 3407

I have removed all the curve settings, set coarse sizes on surfaces and set proximity and curvature refinement with a min size limit of 0.01 and a refinement of 16 (goal of 16 elements in 360) I also added a trailing edge surface all the way back to the far field. You need to set this up as an internal wall (under params by parts) so you get shells to grow prisms on, but then you need to delete those shells before sending to the solver (or put an internal boco on them). I also removed all your initial height settings so that the prism heights could float to give a smoother volume transition between the prisms and the tetras.

Again, the final model was totally periodic

Tet 2 Hex
 

Joel,

One more step...

The last model shown in the previous post had 863K tetras.

I ran the tet to hex conversion (12 to 1) and reduced that to 304K tetras (and 40k hexas).

This has been shown to reduce convergence time by 50% for ducted flow. I don't know of a formal study on wings, but it should help here also.

Attachment 3408

Attachment 3409

Note that fewer size transitions would mean a higher percentage conversion... Also note that you can use density boxes to control where those size transitions take place. Here, I just went with defaults and didn't even create a density region for the wake... In reality, you may want to spend a bit more time in setup to get better mesh control. Also note, that I had to create prisms first. Prisms don't grow well into hybrid mesh because they can't move hexas/pyramids out of the way.

Issues...
 

Blocking...
 

Brian,

Your blocking should look more like this...

Attachment 3421

Note the CGrid out to the boundary (not an H Grid for the Far field and a CGrid around the airfoil for this model). In the end, it is pretty much exactly like my 2D example on www.youtube.com/ansysinc except that you can align the blocking in Z and add an extra split across Z for the wing tip.

I associated all the edges with the airfoil (including at the tip).

I also opened up the airfoil wedge a bit on the opposite far field wall to slightly improve the wedge quality...

The blocking took just a few minutes, but you might spend a few more to get the distributions just right.

Simon

Hi,

I used curve settings instead of surface settings because I was using a patch dependent method and then filling the interior with a delaunay method (let me know if this is the correct way).

I will check my periodic settings, but basically the periodic faces were different when visually inspecting ("view => front"). For the grid without the prismatic layers the mesh was perfectly periodic.

Btw, where do you find the option to run the periodic checks?

Joel

oops.
 

Joel,

Oops, there is the part I missed. The Patch Based Mesher does not respect the periodicity settings, at least not by default. To make it happen, you can mesh the one side, lock all the nodes, copy over to the other side and then mesh the remaining surfaces while respecting line elements... Not the easiest way to handle things. In your case, it worked out ok in the beginning (coincidence) because your curve sizes were all periodic.

But yes, if you want to use Patch Conforming mesh, you need to set the curve sizes.

The Check Periodicity option is under Edit Mesh => Check Mesh.

http://www.cfd-online.com/Forums/att...1&d=1275850954http://www.cfd-online.com/Forums/att...1&d=1275850791Hi Simon,

Here are where the bad elements are, and blocking.

Thanks,

Brian

Quality Improvement
 

I can't really see these elements in this pic, but I can see that they are the trailing edge wedges, both within the solid and the fluid.

First off, you can ignore the poor quality solid elements unless you are doing conjugate heat transfer. If you do need to keep them, the rest below still applies.

You can improve the quality a little on the far side of the fluid by opening up the angle there. The geometry doesn't go all the way, so the mesh doesn't need to be perfectly conformed to that shape all the way either. Open it up to 30 or 60 degrees at the FF using edge splits (not block splits). But this still won't help the elements right at the trailing edge.

Zoom in and take a look at those. The angle is constrained by the geometry, so you can't do anything about that. But if they are really long and skinny (long in the chord direction short across) then perhaps reducing the side 2 mesh size is the best solution to improve aspect ratio. Also look and make sure they don't appear warped or twisted (usually a mis-projection issue or an issue with misaligned edge params).

If your only concern is angle (which you can't possibly fix due to geometry constraints), then I suggest you just send it to the solver and see if the solver is as concerned about it as you are.

Keep in mind that these are just metrics, and some may not align with the needs of your particular solver. The ICEM CFD Quality metric is very "conservative" for prism quality. To calculate the ICEM CFD Quality metric, the software actually divides the prism (Penta-6) into 3 tetras (numerically speaking) and then gives the quality of the worst one. This very conservative metric is needed for some solvers, but not for others.

If you were checking based on "min angle", you would also get a low number, but that would be because it was a prism... The ideal angle for a Hexa is 90 and you really want to stay above 18 or at least 9 degrees for Fluent, but the ideal angle for a prism is 60, and the min angle tolerated by Fluent is much lower.

At 13.0, we are introducing a new "Orthogonal Quality" metric designed by a team of Fluent and CFX developers as the best measure of quality for those solvers.

Hi Simon,

Here is where I am getting angles below 9 degrees. I have tried a few things but no improvement. Any suggestions?

Thanks
Brianhttp://www.cfd-online.com/Forums/att...1&d=1276224400

Ogrid on the inside...
 

This is inside your wing... Do you need to keep the mesh inside your wing for conjugate heat transfer?

This is basically the exact same problem as you had on your far field... The fix is the same also.

If you need the mesh inside your wing (and beyond the wing tip), You must extend your CGrid into your wing and then split the ogrid to capture the surface of the wing. Then collapse three trailing edge blocks. If you don't get it, I can show you...

Another option (I forget your exact topology, so this might not apply) is to sweep unstructured mesh thru the inside of the wing... This would prevent your solid mesh count from getting too high and would be fun to do... Look under "Blocking (tab) => Edit Blocks => Change Block Type" Look for sweep and select the triangular face on the one side.

Simon

sorry the pic is decieving, the elements are actually right on the surface of the wing. Ill try a few things over the weekend.

thanks,

Brian

The elements outside the wing shouldn't have any topology related angle issues... Are you sure these are not right inside where the HGrid corners are opened up to the continuous curve on the inside of the airfoil?

Could you show me how to " If you need the mesh inside your wing (and beyond the wing tip), You must extend your CGrid into your wing and then split the ogrid to capture the surface of the wing. Then collapse three trailing edge blocks. If you don't get it, I can show you..." , thanks a lot.
I am still confused about how to mesh beside the wing tip.

Hi Simon,

You were right, the elements were on the inside of the wing. I tried all the suggestions you mentioned but could not get rid of the low angle elements. Fluent seemed to like the mesh engough to try to solve. Now I will see if I can get a reasonably converged solution.

I can see what splitting edges does(at least along a curved line) but couldnt really tell any difference in the mesh??

Thanks

Brian

Sharp corners of wedges
 

hii I am new to Icem want to mesh one of the part of the object below please give me an idea for blocking of that object.. :confused:

Meshing Wing with round TE problem
 

Hello everybody,

I tried to create the mesh for a wing having the aerofoil NACA23015 and my wing has round trailing edge. I cannot create the mesh at the wing tip ( see attached pictures). Thus, somehow at the walls of the domain, ICEM computed them I must say that my wing does not have a sharp trailing edge.

I followed the tutorial for meshing about a sharp trailing edge and tried to adapt for a round one

Does someone help me with this problem ?

Kind regards,
Andrei